I made some cfd-simulations to get the mass fraction of a species passing a tube inside another type of species. Afterwards I was calculating kind of the ”spread” that the species experienced during this pass. Unfortunately the results differ a lot when I am using different grid types. When I am using a tetrahedral grid the spread is pretty low, when I am using a structured hexahedral grid the spread is about two orders of magnitude higher.
Could this effect arise due to the numerical diffusion within the tetrahedral grid?
We also found out that the larger the diffusion coefficient we are using, the smaller the spread of the species. But within a normal range of variation the difference in the spread of the species is not two orders of magnitude.
Can the effect of the numerical diffusion have such a huge impact on the results of my simulations?
It would be really nice, if somebody could help me!

Does anybody know how I can minimise or (in best case) avoid this numerical diffusion?
I am using the QUICK Scheme know which leads to a much better result, but is there a way to improve the results even more? I thought of maybe reducing the time step size to get a CFL number of about one? Does anybody has experience with this?
Thank you in advance for your help!
Lilly

cfl between 1 and 12
y+ no less than 30 and no bigger than 100, higher or lower values increase the diffusion
timestep as small as possible.
grid must be aligned with the flow, and possibly refined as much as possible where you have the "phase change"
at least second order in space, settle for first order in time, otherwise there might be some instabilities.

take notice that i have never done pipes simulations so the parameters might vary.

Does anybody know how I can minimise or (in best case) avoid this numerical diffusion?

As Sail mentioned, the grid must be aligned with the flow velocity. In my experience, a tetrahedral grid introduces an enormous amount of numerical diffusion. What is the geometry that you are modelling? If it is a simple tube, you should use an extruded grid along the length of the tube.

Unfortunately, my geometry has a bifurcation which makes it really hard to create a structured hexahedral grid aligned with the flow (I tried different mrthods in the bifurcation area, but failed). Do you have any idea how to circumvent this problem?

Unfortunately, my geometry has a bifurcation which makes it really hard to create a structured hexahedral grid aligned with the flow (I tried different mrthods in the bifurcation area, but failed). Do you have any idea how to circumvent this problem?
Lilly

Lilly, for a 2D bifurcation, your meshing strategy should look like the one in the picture. You need to define 3 blocks and then mesh each block with quads. In 3D, the general idea is the same. However, at the sections of each tube you need to use a butterfly-grid. It's fairly straightforward but you have to do the blocking manually.

I'm not sure what program you're using for generating your mesh. I usually use ICEM for these sort of things.